Hide Table of Contents

Hinge Mates

A hinge mate limits the movement between two components to one rotational degree of freedom. It has the same effect as adding a concentric mate plus a coincident mate. You can also limit the angular movement between the two components.

Advantages of hinge mates:
  • When modeling, you need to apply only one mate, where otherwise you would have applied two.
  • If you run an analysis (such as with SolidWorks Simulation), the reaction forces and results are associated with the hinge mate, not one particular concentric or coincident mate.

To add a hinge mate:

  1. Click Mate (Assembly toolbar) or Insert > Mate.
  2. In the PropertyManager, under Mechanical Mates, click Hinge .
  3. Make selections and set options under Mate Selections:
    • Concentric Selections . Select two entities. Valid selections are the same as for concentric mates.

    • Coincident Selections . Select two entities. Valid selections include a plane or planar face and:
      • Plane or planar face
      • Edge
      • Point

    • Specify angle limits. Select to limit the angular rotation between the two parts. Define the extent of rotation:
      • Angle Selections . Select two faces.

      • Angle. Specify the nominal angle between the two faces.
      • Maximum Value
      • Minimum Value
  4. Click .

    Hinge appears in the Mates folder in the FeatureManager design tree.

    For more information, see SolidWorks Help: Mates Overview.

Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Hinge Mates
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: SOLIDWORKS 2011 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.